ECE101 – Basic Electrical and Computer Engineering

Creating Devices in EAGLE Part II – The Symbol and Device

For those who watch only the video, please also read the first paragraph as it has a few notes that I didn’t cover in the video.

Having created the package for the 2.5 Digit LCD in the last post, I’ll be creating the corresponding symbol and device in this post.  You can have more than one package associated with a symbol in one device.  You can also use the same package over in other devices in association with their respective devices.  So when creating a standard package, like a TSOP or QFP, it would be best to give it a more generic name, such as TSOP-44, so you can use it with other devices.  Also, for those wanting to have the names and values on either the package or the symbol, just add the text “>NAME” and “>VALUE” (without the quotes of course) to your symbol and/or package.

The Symbol

To create the symbol, click the Symbol button on the top toolbar from any window within your library.  When prompted for a name, enter an appropriate name for the symbol (I used 2.5_DIG_LCD), click Ok, and then click Ok to again to confirm that you want to create a new symbol.  This will bring you to a window heavily resembling that of the schematic window.

To start creating the symbol, there are a few things to note on the datasheet.  The first is that this particular device has 16 signal pins, one of which is a common pin.  Common practice for creating symbols is to have the power pins on top, grounds on bottom, inputs on the left, and outputs on the right.  Since the common pin can be either power or ground, the other fifteen pins can be considered either inputs or outputs, depending on the selection for the common pin.  For this reason, I’ll be putting the common pin on one side (as it can be considered as the opposite – input or output – of the other fifteen pins), and the fifteen signal pins on the other side.

To place pins, select the pin tool and begin placing them on the page.  The order on the symbol isn’t so important as their is no physical meaning to the order of the pins.  I placed fifteen pins on the right and one on the left with enough space between the two sides to clearly display the pin names.  For the fifteen pins on the right, I placed them one grid space apart.  This helps to keep the symbol reasonably sized in comparison to other symbols you’ll be placing on your schematic.  As with the order, there is no physical meaning related to how far apart they are, it just helps keep the symbol size reasonable.

After the pins have been placed, I draw a box (using the Wire tool) so I can tell which pins go together once a part is placed in a schematic.  This may seem trivial, but I recently inherited a schematic that has a dozen pins just floating in the schematic.  You can’t tell which pins go together just by looking, so the first thing I’ll be doing is recreating those symbols.

With the pins placed, now they just need to be given names.  Select the Name tool, and give each pin a name corresponding to a signal from the datasheet.  If you did this on the package as well (sorry, I didn’t), it makes connecting the package and symbol very straightforward.

Finally, to have the name display on the schematic, use the text tool and place “>NAME” on your symbol.  This can be done on the package as well so that the name will come out in the silkscreen.  Though this part doesn’t have a value like a resistor or capacitor, the text “>VALUE” will display any values you set.

The Device

The last step is creating the device by combining the package and symbol.  Click Device on the top toolbar, enter a name and press Ok.  In the device window, click Add on the left toolbar and add the symbol you just created.  In the lower-right corner, click New and select the package you created.  Finally, click Connect to display the connection dialog.  If you named all of the pads in your package and all of the pins in your symbol, you just need to click connect 16 times.  If you didn’t, you need to make sure that you connect the right pad to the right pin; otherwise you’re schematic will look correct, and your board will seem correct, but it won’t work the way you expect it to.

Congratulations

If you’ve gone through the previous posts, you should be able to use the basic features of EAGLE to create quite an array of boards.  Some boardhouses will even take your board files to create your boards, taking the task of creating gerber files off your shoulders.  However, since a lot of people use boardhouses that require gerbers, including myself, my next post will be a tutorial on creating gerber files.  Until then, tell me what areas you need help with, and I’ll be sure to include them in my upcoming posts.